Sketcher CATIA Training Foils Version 5 Release 9 June 2002

Sketcher CATIA Training Foils Version 5 Release 9 June 2002
EDU-CAT-E-SKE-FF-V5R9 Copyright DASSAULT SYSTEMES 2002

Course Presentation Objectives of the course Targeted audience
In this course you will learn how to sketch, constrain, and edit 2D profiles. These profiles are then used to generate solids and surfaces Targeted audience New users Prerequisites CATIA Basics 1 day Copyright DASSAULT SYSTEMES 2002

Table of Contents (1/3) Introduction to CATIA Sketcher p.6
Workbench Presentation p.7 Sketching Simple Profiles p.17 The Sketcher Work Modes p.18 Profiles p.26 Points p.29 Lines p.33 Spline p.37 Circles and Arcs p.41 Conics p.47 Axis p.53 Sketching Pre-Defined Profiles p.57 Sketching Pre-Defined Profiles p.58 Editing Profiles p.64 Modifying Profile Geometry p.65 Editing a Spline p.70 Copyright DASSAULT SYSTEMES 2002

Table of Contents (2/3) Operations on Profiles p.75
Re-Limiting Operations p.76 Transformation Operations p.88 Offset p.94 Operation on 3D Geometry p.99 Edit Mark Definition p.105 Editing Parent Children and Constraints p.108 Setting Constraints p.111 Introduction to Constraints p.112 Quick Constraints p.117 Constraints Via Dialog Box p.123 Auto Constraints p.126 Animating Constraints p.131 Sorting Sketches by their Solving Status p.132 Relation between Dimensions p.137 Copyright DASSAULT SYSTEMES 2002

Table of Contents (3/3) Managing Sketches p.141 Creating Planes p.142
Replacing a Sketch p.149 Changing Sketch Support p.150 Sketch Analysis p.153 Change Body p.164 Copyright DASSAULT SYSTEMES 2002

Introduction to the CATIA Sketcher
In this lesson you will see the V5 CATIA Sketcher user interface and basic functions Why Using the Sketcher ? Discover It Sketcher Workbench Sketcher Interface Sketcher Terminology Sketcher General Process To Sum Up Copyright DASSAULT SYSTEMES 2002

Why Using the Sketcher? The Sketcher is a set of tools to help users quickly generate 2D Geometry. The completed Sketch can then be used to generate Solids and Surfaces The capability to define Constraints between elements in the Sketcher allows for quick modification of the Sketch and consequently the Solids or Surfaces that are based on it. Other tools such as Animate Constraints enable the user to explore design alternatives Copyright DASSAULT SYSTEMES 2002

Sketcher Workbench (1/2)
Select Start > Mechanical Design > Sketcher then select a plane or a face on an object Copyright DASSAULT SYSTEMES 2002

Sketcher Workbench (2/2)
You can also access the Sketcher by selecting the Sketcher icon from any Workbench where it is possible to do a sketch. If you want to create a Sketch by specifying its 3D position and orientation, you have to select the Sketch Positionning icon. A dialog box where you can define the Absolute Axis System appears. If you create a Sketch, it will be positionned regarding to this System. Copyright DASSAULT SYSTEMES 2002

Sketcher Interface (1/4): Sketcher Workbench General
A New Sketch will register in the Part Tree when entering the Sketcher Workbench Standard tools Exit to 3D Space Part tree Tools & Operations Constraints Icons New Sketch Sketcher Design tools... Copyright DASSAULT SYSTEMES 2002

Sketcher Interface (2/4): Sketcher Tools
Exit Sketcher Profile Rectangles, Polygons... Circles, Ellipse, Arcs... Spline Ellipse Line Axis Points... Corner Chamfer Trim options... Symmetry Projection Constraints dialog box Constraint Auto Constraint Animate Constraint Profiles Operations Constraints Copyright DASSAULT SYSTEMES 2002

Sketcher Interface (3/4): Toolbars
Icons Insert menu or toolbars Predefined Profiles Circles Conic Line Point Copyright DASSAULT SYSTEMES 2002

Sketcher Interface (4/4): Sketcher Plane
It is possible to zoom, pan and rotate (using the mouse). To reset a sketch plane orientation, select the Normal View icon Once on the plane on which you want to sketch has been selected, it is displayed parallel to the screen (if Tools+ Option + mechanical Design + Sketcher + Position sketch plane parallel to screen is active) If you select the Normal View icon when the sketch plane is already displayed parallel to the screen, you will turn the sketch plane and see its other side. Copyright DASSAULT SYSTEMES 2002

Sketcher Terminology The Sketch is the holding point for a group 2D elements on a specific plane. There can be more than one Sketch using the same plane as support. The V-H Axis is the 0,0 for the Sketch. Sketches generally consist of a Profile, Constraints, and Dimensions (a type of Constraint). Profile Constraints Dimensions Copyright DASSAULT SYSTEMES 2002

General Process 1 2 3 4 5 6 Access the Sketcher workbench
Select a plane, a solid face, or a planar surface to sketch on Access the Sketcher workbench 3 An in-work sketch is added to the Specification tree 4 Create geometric elements 5 Constrain the geometric elements Use the sketch to create a solid or surface 6 Copyright DASSAULT SYSTEMES 2002

You have seen: To Sum Up A “QuickStart” Sketcher demonstration
Why Sketch? How to access the workbench Its user interface and tools The terminology that will be used The general design process Copyright DASSAULT SYSTEMES 2002

Sketching Simple Profiles
In this lesson you will learn how to create most of the Sketcher geometric elements. You will also learn how to use the various work modes available for the Sketcher Workbench The CATIA Sketcher Work Modes Profiles Points Lines Splines Circles and Arcs Conics Axis To Sum Up Copyright DASSAULT SYSTEMES 2002

The CATIA Sketcher Work Modes
You will learn the Sketcher work modes by using: Grid/Snap Standard/Construction Geometry Value Fields Automatic Constraints Automatic Dimensions Section View Copyright DASSAULT SYSTEMES 2002

Why Sketcher Work Modes?
The Sketcher work modes aid you while you sketch the geometry. They facilitate input of values, automate Geometrical/Dimensional Constraints creation, help visualize 3D geometry etc ... Copyright DASSAULT SYSTEMES 2002

Using Grid/Snap When creating any lines ( profile, segment, circle, arc, curve, …), you can activate or deactivate the snap to point icon at any time. When the snap to point icon is active, the cursor only snaps on the points of the grid (graphical creation). If you enter coordinates when the snap to point icon is active, the system does not take into account the grid and place the point in accordance with the coordinates you have entered. To modify the grid parameters, select Tools + Options… from the top of the screen, select Mechanical Design from the dialog box then, select the Sketcher tab. 3 1 5 4 2 Copyright DASSAULT SYSTEMES 2002

Standard / Construction Geometry
Two types of element: Standard or Construction Standard elements represent the most commonly created elements Construction elements aim at helping you in sketching the required profile. They facilitate your design Creating standard or construction elements is based upon the same methodology. Clicking the icon switches from one mode to the other Standard + Construction Elements Copyright DASSAULT SYSTEMES 2002

Value Fields When sketching, you can enter exact coordinates/lengths/angles in the Tools bar. 1 For the profile first point, you can define the Horizontal and Vertical coordinates. By pressing the tab key you access the Horizontal coordinate field, so you can enter it. By pressing the tab key once more, you access to the Vertical coordinate field, so you can enter it For example, in using the Profile tool ... 2 For the profile second point, you can also use the tab key to enter a coordinate, but you can also define the second point of the profile by entering the length of the segment between the first and the second point and/or by entering the angle between the Horizontal axis and the segment to be created. 3 When profiling an arc, the tools bar allows you to enter the H and V coordinates of the last point of the arc but you can also enter a radius. You can enter these coordinates by using the tab key. If you enter only one of the coordinates (H, V, L, A or R) you fix it, this means that the other parameters can move graphically but not the fixed one. Copyright DASSAULT SYSTEMES 2002

Automatic Dimensions 1 2 3 4 When activated:
- corner dimensions - chamfer dimensions - dimensions entered into the value fields are automatically created during geometry construction. Multi-select two edges of existing rectangle In sketcher, select the Dimensional Constraints Icon 2 3 Select the Corner icon 4 Move the corner preview to the desired location and click With Dimensional Constraints on With Dimensional Constraints off Copyright DASSAULT SYSTEMES 2002

Automatic Constraints
In sketcher, select the Geometrical Constraints Icon 1 2 In Tools/Options/Mechanical Design/Sketcher/Constraint/SmartPick specify which Constraints you want detected Notice that Tangency Constraints are created even if Geometrical Constraints is Off With Geometrical Constraints Off 3 Start to sketch the geometry. Variations of valid Constraints will be proposed depending on where the Mouse is with respect to the existing geometry. When you see the Constraint you require, click on the Mouse to store the Constraint (and the new geometry). With Geometrical Constraints On Copyright DASSAULT SYSTEMES 2002

Section Views In order to see a Section View of the part while sketching, click on the Cutting Plane icon in the Cut By Plane toolbar. This is purely a visualization tool, no intersection curves are created from the intersection of the Solid with the Cutting Plane. If you need to constrain to (or Dimension off from) the intersected outline of the Solid, use the Intersect 3D Elements tool Copyright DASSAULT SYSTEMES 2002

You will learn how to create a Profile element
Profiles You will learn how to create a Profile element Profile in the Sketcher Profile seen in 3D Copyright DASSAULT SYSTEMES 2002

What are Profiles ? A profile is a series of adjacent planar geometric elements such as points, lines, and curves Profiles are used to extrude Sketch-Based features Closed or open ? A profile can be: "Closed" (the last element connects up with the first element in the series) or "Open" (the first and last elements in the series are not in contact). If a profile is "Closed", it can have other profiles contained inside its boundaries Open profile Inner profiles A profile, within a profile, is shown here to illustrate how "Inner Domains" work. Notice the reversals of the Boolean operations between addition and subtraction as we progress from the outside inwards Inner profiles Copyright DASSAULT SYSTEMES 2002

Select the tangent arc icon, select end point
Creating Profiles 3 Tangency constraint Horizontal constraint 1 In the Sketcher, Select Profile icon 2 Select the line icon (default) and click on two points to create line Select the Three Point Arc icon and click on two points to create arc 6 4 Drag horizontally and click to create line. Rather than using the Tangent arc icon to create the final arc, click, drag and release at the beginning of the arc and CATIA goes into the tangent arc mode automatically. 5 Select the line icon and drag vertically to create line and click Copyright DASSAULT SYSTEMES 2002

You will learn the various methods to create points
Copyright DASSAULT SYSTEMES 2002

Two Ways to Create Points in the Sketcher
Points can be created in the Sketcher in two ways: - By the user - By the system When the user creates a line, the line’s end points are automatically created by the system. When the user creates a circle, the center point is created. The coordinates of these automatically created points can later be modified by double-clicking and entering new values. Alternatively, the user can first create the points directly. He can then create a line or any other geometry by selecting these points. Copyright DASSAULT SYSTEMES 2002

Points by Identification
1 2 Click to define the location where you want the point In the Sketcher, select the Point by clicking on the Coordinates icon For ease of placing the points, select the Snap to Point icon so the cursor will snap to the grid while trying to locate the point Copyright DASSAULT SYSTEMES 2002

Points by Coordinates 1 Fill in the desired Cartesian or Polar coordinates In the Sketcher, select the Point by clicking on the Coordinates icon 2 If the Dimensional Constraints mode is on, Polar dimensions will automatically be created in the case of Polar input. (Cartesian dimensions created in the case of Cartesian input) Copyright DASSAULT SYSTEMES 2002

You will learn the various methods to create lines

What is a Line in CATIA V5? In CATIA V5, a line segment is described in the Specification Tree by three nodes - two point nodes (Point.1 and Point.2) and one line node (Line.1). The line is supported by its parents - the points. When the position of a point is modified (either by double-clicking and entering new coordinates; or by dragging), the position of the line will change accordingly. Copyright DASSAULT SYSTEMES 2002

Lines Between Two Points
1 2 Click on starting point of the line... …then click on the end point In the Sketcher, select the Line icon 3 OR… you can type the line specifications in the value fields of the Tools toolbar Copyright DASSAULT SYSTEMES 2002

Bi-Tangent Lines 2 1 Select the two elements you want the line to be tangent to ... In the Sketcher, select the Bi-Tangent Line icon The Bi-Tangent line is created Copyright DASSAULT SYSTEMES 2002

You will learn how to create a Spline in the Sketcher
Splines You will learn how to create a Spline in the Sketcher Copyright DASSAULT SYSTEMES 2002

Which Should I Use - Sketcher Spline or 3D Spline?
Since the 3D Spline Tool - available within the Wireframe&Surfaces (WFS) or Generative Shape Design (GSD) workbenches - can also be used in a 2D manner (with Geometry on Support being a plane), when should you use the Sketcher Spline and when is the 3D Spline more appropriate? In general, use the Sketcher Spline to create Sketches for generating solid Sketch-Based Features. (Although Pads and Pockets can be generated from 3D Splines) Use the 3D Spline when you need more control over the Spline - i.e. Tangent Tension, Curvature Direction, Curvature Radius. Surfaces can be generated from Splines created by either method. Copyright DASSAULT SYSTEMES 2002

Creating a Spline 1 3 2 …then click the second point of the spline Click first point to start the spline In sketcher, select the Spline Icon 5 Double-click to specify the spline End Point. 4 4 Double-Click on a Spline Control Point to specify exact coordinates or to create a Tangency vector at that point. You can later apply Constraints to this vector (i.e. make it parallel to a line). …then click for the third point of the spline Double-click on a Spline Control Point to specify exact coordinates or to define a Curvature after a tangency vector Copyright DASSAULT SYSTEMES 2002

Connecting Curves 1 2 3 Select the Connect icon Select the first curve
Select the second curve You get: Copyright DASSAULT SYSTEMES 2002

You will learn the various methods to create circles and arcs.

What are Circles and Arcs in CATIA ?
In CATIA V5, a Circle consists of two nodes: Point specifying the coordinates of the Circle Center Circle.1 specifying the Radius of the Circle The Arc will have two additional nodes: Point specifying the coordinates of one limit Point specifying the coordinates of the second limit Note: When a Circle is Trimmed leaving only a portion of the complete circle. Two additional points are added to the Specifications Tree. In fact, the representation becomes the same as that of an Arc. Copyright DASSAULT SYSTEMES 2002

Basic Circles 1 Click once to define the center point of the circle, then drag the cursor 2 In the sketcher, select the Circle icon 3 …and click again to define the circle size Copyright DASSAULT SYSTEMES 2002

Circles Through Three Points
1 Click three times to define 3 points. The circle will pass through these points 2 In the Sketcher, select the Three Point Circle icon 3 4 Copyright DASSAULT SYSTEMES 2002

Circles Using Coordinates
1 In sketcher, select Circle using the Coordinates icon 3 2 Enter the size of the radius Enter the absolute coordinates of the circle Copyright DASSAULT SYSTEMES 2002

Three Points Arcs Click to define the first point to start the arc... 1 2 In the Sketcher, select Three Point Arc icon 3 …then click to define the second point of the arc 4 Then click to define the end point of the arc Copyright DASSAULT SYSTEMES 2002

You will learn the various methods to create conics

Types of Conic that Can Be Created
Ellipse Parabola Hyperbola Conic Required Inputs Ellipse Center, Major Axis Limit, Point on Curve Parabola Focus, Apex, Start Point, End Point Hyperbola Focus, Center, Apex, Start Point, End Point Copyright DASSAULT SYSTEMES 2002

Creating an Ellipse (1/2)
Click to indicate center point of ellipse 3 2 …then click the second point for the major axis endpoint 1 In the Sketcher, select the Ellipse Icon The Tools Toolbar then displays values for defining the ellipse major axis endpoint Center point coordinates can also be input in the Tools Toolbar Copyright DASSAULT SYSTEMES 2002

Creating an Ellipse (2/2)
4 Click to indicate for minor axis endpoint Copyright DASSAULT SYSTEMES 2002

Creating a Parabola Click to indicate the Focus Point of the Parabola 2 …then click the second point for the Apex 3 1 In the Sketcher, select the Parabola Icon 4 Next indicate the two endpoints As always, the Tools Toolbar is contextual and allows the user to input specific point coordinates during the creation steps Copyright DASSAULT SYSTEMES 2002

Creating a Hyperbola Click to indicate the Focus Point of the Hyperbola 2 4 … click the third point for the Apex 1 In the Sketcher, select the Hyperbola Icon Next indicate the two endpoints 3 …then click the second point for the Center 5 As always, the Tools Toolbar is contextual and allows the user to input specific point coordinates during the creation steps Copyright DASSAULT SYSTEMES 2002

You will learn the method to create an Axis in Sketcher

What is the Axis Used for?
An Axis element must be included in a Sketch from which a Shaft or Groove solid feature is created. The Profile to be swept around this axis must either be Closed or have its endpoints Coincident to the axis. An Axis drawn into a Sketch can also be used (but not required) to generate a Surface of Revolution. A separate Line or Solid Edge can also serve to specify the axis of revolution. Also, the Profile need not be Closed nor Coincident to the axis in this case. Copyright DASSAULT SYSTEMES 2002

Creating an Axis 1 2 Click the first location for starting point of the axis... In the Sketcher, select Axis icon …then click the end location You will need axes whenever using a symmetry command or creating a grove or shaft. 3 Using the shaft command on our profile sketch, CATIA produces a shaft using the axis we defined Axes cannot be converted into construction elements Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have seen how to set the Sketcher work modes:
Grid/Snap Construction/Standard Elements Automatic Constraints and Dimensions etc … You are now familiar with tools for Sketching simple profiles: Profile Points Lines Splines Circles and Arcs Conics Axis Copyright DASSAULT SYSTEMES 2002

Sketching Pre-Defined Profiles
In this lesson you will learn how to Sketch the Pre-Defined Profiles Sketching Pre-Defined Profiles To Sum Up Copyright DASSAULT SYSTEMES 2002

Sketching Pre-Defined Profiles
You will learn the different ways to create pre-defined profiles Rectangle Oriented Rectangle Parallelogram Elongated Hole Cylindrical Elongated Hole Keyhole Profile Hexagon Copyright DASSAULT SYSTEMES 2002

What are Pre-Defined Profiles ?
Pre-Defined Profiles are tools to facilitate the creation of standard complex shapes with the minimal number of inputs that can fully describe all aspects of that shape. It increases productivity by reducing Mouse/Keyboard interactions Copyright DASSAULT SYSTEMES 2002

Rectangle 1 Click to define the starting corner of the rectangle... 2 …then click to define the diagonal corner In the Sketcher, select the Rectangle icon 3 OR… you can type the rectangle specifications in the value fields of the Tools toolbar In creating all the Pre-Defined Profiles, it is always useful to read the prompts at the bottom left corner of the screen Copyright DASSAULT SYSTEMES 2002

Parallelogram 3 1 2 4 …then click to define the second corner
Click to define the starting corner of the Parallelogram ... … finally, click to determine the width and internal angles of the Parallelogram In the Sketcher, select the Parallelogram icon OR… you can type the Parallelogram specifications in the value fields of the Tools pallet Copyright DASSAULT SYSTEMES 2002

Elongated Hole 3 2 4 1 … indicate the second center ...
Indicate the first center of the hole ... … finally, click to determine the radius of the Elongated Hole In the Sketcher, select the Elongated Hole icon OR… you can type the hole specifications in the value fields of the Tools pallet Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have learned to create Pre-Defined Profiles such as:
Rectangle Oriented Rectangle Parallelogram Elongated Hole Cylindrical Elongated Hole Keyhole Profile Hexagon Copyright DASSAULT SYSTEMES 2002

Editing Profiles Modifying Profile Geometry To Sum Up
In this lesson will learn tools to help you edit Sketcher elements Modifying Profile Geometry To Sum Up Copyright DASSAULT SYSTEMES 2002

Modifying Profile Geometry
You will learn how modify 2D sketch elements to propagate changes to 3D parts Before After Change Copyright DASSAULT SYSTEMES 2002

Why Modify Profile Geometry?
Sketch-based features rely on profiles for their shape Especially if defined with the proper constraints that represent the design intent of the part, the profile geometry can easily be changed for downstream design changes Modified cube Corner removed from sketch Design change Changing the sketch that defines a feature propagates that change to all subsequent operations involving the feature Copyright DASSAULT SYSTEMES 2002

Modifying Profile Element Coordinates
Double click the line to edit its coordinates 1 2 Edit the existing coordinates of the line to new parameters (V: 50mm) H: -40 V: 50 This method works on most construction entities, opening the appropriate dialog for the entity selected Copyright DASSAULT SYSTEMES 2002

Editing Profile Shape and Size
1 Click and drag the line downward to its new location The profile changes according to where you move the element and the constraints you have applied 2 You have modified the shape of the profile without using any intermediary menu options Copyright DASSAULT SYSTEMES 2002

Deleting Sketcher Elements
Select the element to delete 1 Select Edit->Delete and the element is suppressed. Now multi-select additional elements to delete 2 Use the contextual menu (select Mouse Button 3 while cursor is on one of the selected elements) to delete 3 Select the Undo icon or option to restore deleted elements. The Undo icon or option will remember all changes up to the last time the part was saved Copyright DASSAULT SYSTEMES 2002

Editing a Spline (1/3) You can edit a spline modifying, adding or removing the spline control points 1 Double click on the spline to be edited 2 Select the control point to be edited You will see: 3 Copyright DASSAULT SYSTEMES 2002

Editing a Spline (2/3) 4 5 6 Select the control point to be edited
Select the Add Point After option 6 Click a point You will see: Using the same method, you can add a point before the current point or to replace the current point by another one Copyright DASSAULT SYSTEMES 2002

Editing a Spline (3/3) You can also close the spine
You can also define a tangency or/and a curvature on the current point Do not forget to select OK in the dialog box to validate the modifications Copyright DASSAULT SYSTEMES 2002

Auto Search Commands such as Auto Search that are found in the Menu bar can be added as an Icon into a Toolbar if desired 1 Select one element in the Profile Drag down to Auto Search from the Edit Menu bar. All elements in the Profile are selected. 2 Auto Search is a multi-selection tool. Once selected, you can use the Contextual menu to delete or change the properties of all the elements in one go. Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have seen various ways you can edit Profiles:
Double-Clicking to edit Element Coordinates Modifying Shape and Size by Dragging Deleting Elements and Using Auto-Search as a handy tool for Multi-Selecting a Profile Copyright DASSAULT SYSTEMES 2002

Operations on Profiles
In this lesson you will learn how to reuse existing geometry Re-Limiting Operations Transformation Operations Offset Operations on 3D Geometry To Sum Up Copyright DASSAULT SYSTEMES 2002

Re-Limiting Operations
You will learn how to re-limit geometry using Corner, Chamfer, Trim, and Break Operations Before Relimitations After Relimitations Copyright DASSAULT SYSTEMES 2002

Why Re-Limiting Geometry?
In general, there is much less need to re-limit geometry in V5. Each one of the closed profiles below was completely sketched with a single activation of the Profile tool. (Refer back to the Profile section for help in sketching these profiles) In fact, using the Profile tool whenever possible is the preferred practice since it will cut down on the number of user interactions. For a large number of cases, however, re-limitation of sketched geometry using Trim or Break is still necessary to achieve Design Intent. Copyright DASSAULT SYSTEMES 2002

Corners Select the Mode - Trim All, Trim First Element, or No Trim 2 Select the Corner Icon 1 3 Select the two lines 4 Move the mouse around so that the corner is visualized in the correct quadrant 5 Type in the radius required and hit Enter If Dimensional Constraints is activated , the radius dimension will be created on the Sketch. Copyright DASSAULT SYSTEMES 2002

Chamfers (1/3) The chamfer command allows you to create a chamfer between two lines trimming either both, the first or none of the elements 2 Select the first line on which the chamfer will be created 3 1 Select the Chamfer icon Select the second line on which the chamfer will be created Select the desired chamfer trim option 4 5 Select the desired chamfer definition option You get: 6 Using the TAB key, enter the chamfer parameters 6 Press the Enter key to validate the chamfer creation Copyright DASSAULT SYSTEMES 2002

Chamfers (2/3) Chamfer trim options a a a b b b Trim all elements
Trim first element No trim Copyright DASSAULT SYSTEMES 2002

Chamfers (3/3) Chamfer definition options Length/Angle option:
Length1/Length2 option Length1/Angle option: Copyright DASSAULT SYSTEMES 2002

Trimming Lines (1/5) Use the trim icon to keep/erase segments before or after an intersection point between two curves or lines According to the selected trim option (Trim All or Trim First Element), you will get : 2 Select the lines you want to trim on the sides you want kept. 1 Select the Trim icon Trim all elements Trim the first element Move the mouse around before selecting the second line - notice that the system shows you the various solutions possible depending on where you select this line. Copyright DASSAULT SYSTEMES 2002

Trimming Lines (2/5) - Quick Trim
Using Quick Trim when trimming lines and curves, allows you quickly remove unwanted segments 3 Select the line (a) to be trimmed You get : 2 Select the Quick trim option Deletes 1 Select the Quick Trim icon You get : Keeps You get : Breaks Copyright DASSAULT SYSTEMES 2002

Trimming Lines (3/5) - Close
Using Close allows you to close an arc into a full circle. 1 Select the Close icon 2 Select the arc to be closed You will get : Copyright DASSAULT SYSTEMES 2002

Trimming lines (4/5) - Close
You can close an opened ellipse using the Close icon 1 Select the Close icon from the Operation toolbar Select the part of the ellipse you want to close 2 3 You get: Copyright DASSAULT SYSTEMES 2002

Trimming lines (5/5) - Close
You can also close an opened ellipse using the contextual menu of the ellipse 1 Select the Close command from the ellipse contextual menu (MB3) 2 You get: Copyright DASSAULT SYSTEMES 2002

Breaking (a) (b) Use Break to split a line or curve into two parts. 1
Select the Break icon 2 Select the line to be broken (a) then select the breaking line (b) You will get two lines (L1 and L2) : (a) (b) Copyright DASSAULT SYSTEMES 2002

Transformation Operations
You will learn how to perform transformations such as Rotation, Translation, Scaling and Symmetry on Sketcher Geometry 7 X 45 Degrees Rotation in Duplicate Mode Copyright DASSAULT SYSTEMES 2002

Why Transform Geometry?
Using Transformations helps the user avoid repetitive work by enabling the user to reuse existing geometry to help define new geometrically-related Sketcher elements. Copyright DASSAULT SYSTEMES 2002

Symmetry 2 1 3 Select the Symmetry icon
Select (or Multi-Select) the element(s) to symmetrize Remember that there are a variety of Multi-Selection Tools available 3 Select a line or axis to specify the axis of symmetry Copyright DASSAULT SYSTEMES 2002

Translation In general, once a value is entered, it is temporarily fixed. The remaining values continue to float. In the example below, if the length of translation is entered, the user is still capable of moving the mouse around to change the direction of the translation. Number of Copies 1 Select (or Multi-Select) the element(s) to translate 2 Select the Translation Icon Select a first point on the Grid to define the origin of the translation 3 4 Options: A) Select a second point of the Grid to define the distance and direction for the translation B) Type in the coordinates of the second point into the Tools Toolbar C) Make the Translation Definition window active and type in the Length of translation. Indicate the preferred direction. (Press the TAB key to go between fields) Copyright DASSAULT SYSTEMES 2002

Rotation When the Snap Mode is active (as in the Rotation Definition window), the angle values that are proposed as the user moves the mouse around will take on Integer increments 1 Select (or Multi-Select) the element(s) to rotate 2 Select the Rotation Icon Select the Center Point for the Rotation 3 4 Options: A) Select two points on the Grid with respect to the center to define the angle B) Type in the coordinates of the two points into the Tools Toolbar C) Make the Rotation Definition window active and type in the Angle of Rotation (Press the TAB key to go between fields) Copyright DASSAULT SYSTEMES 2002

Scaling When the Duplicate Mode is not active, the selected geometry is transformed (no new elements are created) 1 Select (or Multi-Select) the element(s) to scale 2 Select the Scaling Icon 3 Options: A) Select the Center Point and a second point on the Grid with respect to the center to define the magnitude of the Scaling B) Type in the coordinates of these two points into the Tools Toolbar C) Select a center point. Make the Scale Definition window active and type in the Scaling Factor (Press the TAB key to go between fields) Copyright DASSAULT SYSTEMES 2002

You will learn how the Offset tool is used

What is the Offset Operation?
Offset is a local operation which allows you to duplicate one or several elements of a profile. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones The offset can be positive or negative to determine on which side of the profile the offset profile will be created Copyright DASSAULT SYSTEMES 2002

Offsetting Elements (1/2)
The Offset capability allows you to duplicate one or several elements in the Sketcher. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones 1 Once in the Sketcher, select one of the element to be offset 2 Select the Offset icon 3 In order to select the connected element of the profile, select the Point Propagation icon Copyright DASSAULT SYSTEMES 2002

Offsetting Elements (2/2)
The Offset command allows you to duplicate one or several elements in the Sketcher. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones 4 In the Tools toolbar, enter the Offset value: 2 You get: 5 Press the Enter key 6 To validate, click on the side you want to get the offset profile Copyright DASSAULT SYSTEMES 2002

Additional Information
Different options to define an offset Instead of entering an offset value, you can define a point the offset profile will pass through by entering its coordinates To offset only the selected element To define several instances To offset only in both directions To offset only the tangent elements Copyright DASSAULT SYSTEMES 2002

Operations on 3D Geometry
You will learn what tools operate on 3D Geometry from Sketch Mode and why they are important Copyright DASSAULT SYSTEMES 2002

What are the Tools that Operate on 3D Geometry and Why are they Important?
Project - projects elements that are off the current Sketch plane into the Sketch. - Projection is associative to the parent 3D geometry Intersect - intersects 3D elements with the Sketch plane - Intersection is associative to the parent 3D geometry Isolate - Breaks the links that Projected and Intersected elements have with their parent 3D geometry so that they may be edited independently The Profile of the Tray is linked to the Profile of the Support through a Projection Tray Support Copyright DASSAULT SYSTEMES 2002

Project 3D Elements 2 1 Select (or Multi-Select) the elements to project onto the Sketch plane. (Selecting Solid Faces or Surfaces will project the boundary curves of these elements) Select the Projection Icon Here … a projected Solid Edge (a Spline contour) is used as part of the closed profile for the current Sketch Copyright DASSAULT SYSTEMES 2002

Intersect 3D Element Select (or Multi-Select) the elements to intersect with the Sketch plane. Select the Intersection Icon 1 2 If the shape of the surface should change, this contour will also change accordingly Here … the curve generated by intersecting the surface with the Sketch plane can be used as part of the closed profile for the current sketch Copyright DASSAULT SYSTEMES 2002

Project 3D Silhouette Edges
The Project 3D Silhouette Edges command shows how to create silhouette edges to be used in sketches as geometry or reference elements. Limitations are the same as for the Projection/Intersection tool, as far as associativity is concerned. You can only create a silhouette edge from a canonical surface whose axis is parallel to the Sketch plane. Select the Project 3D Silhouette Edges icon Select the element to be projected 2 1 You get: Copyright DASSAULT SYSTEMES 2002

Isolate The Isolate command breaks the links between Projected and Intersected elements and their parents 3D geometry so that they may be edited independently Activate the Isolate option from the menu - Insert/Operation/3D Geometry 2 1 Select (or Multi-Select) the elements to be isolated (Here … two of the edges from the projected face) The isolated lines turn white to indicate that they are no longer linked. You can now drag these lines to new locations or change them as needed A Projected or Intersected curve does not need to be isolated in order to be re-limited (position is not modified) Copyright DASSAULT SYSTEMES 2002

Edit Mark Definition You can see the mark characteristics and you can transform the mark into a construction element. The mark can result from a projection or an intersection 2 In the dialog box, select the Construction element button 3 Select OK 1 In the Sketcher, double click on the projection You get: The mark is now a construction element Copyright DASSAULT SYSTEMES 2002

Edit and Modify Import Properties (1/2)
You can edit Projections and Intersections 1 Double click on Projection.4 2 Select a new edge to be projected, then select OK New edge When leaving the sketcher, you will get: Double click Copyright DASSAULT SYSTEMES 2002

Edit and Modify Import Properties (2/2)
You can highlight the Reference Element inside the Sketch. 1 Project your Line onto the plane. 2 If you double click on this projection, the Reference Element will be highlighted. Copyright DASSAULT SYSTEMES 2002

Editing Parents Children and Constraints (1/2)
You can edit an element using the Parents/Children capability Select Parent/Children from the constraint contextual menu 1 2 Select Show All Parents from Offset.12 Copyright DASSAULT SYSTEMES 2002

Editing Parents Children and Constraints (2/2)
3 Select Edit from Pad.1 You can, now, edit the pad Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have learned how to perform various operations on
the geometry you create in the Sketcher (and to bring 3D geometry into the context of the Sketcher): Re-limiting Operations (Corners, Chamfers …) Global Transformations (Translations, Rotations …) Offset Operations on 3D Geometry (Project, Intersect …) Copyright DASSAULT SYSTEMES 2002

Setting Constraints Introduction to Constraints Quick Constraints
In this lesson you will see: Introduction to Constraints Quick Constraints Modification of Constraints Auto Constraints Animating Constraints Sorting Sketches by their Solving Status Relations Between Dimensions To Sum Up Copyright DASSAULT SYSTEMES 2002

Introduction to Constraints
You will learn the different ways to create constraints What are Constraints and why do we need them? Sketching in Context Copyright DASSAULT SYSTEMES 2002

Movement of 4 Unconstrained Lines
Why Constraints? Without Constraints, geometry can be moved freely just by using the mouse to drag them. If Sketcher profiles are moved, so do the solids that are supported by them. In the context of an assembly, if one part moves, another part that is related to it may also move. Although in CATIA V5 geometry will remain in place when put there, without Constraints any subsequent movement of elements by the user may go unnoticed and affect Form Fit and Function of entire assemblies. Hence, Constraints serve to mathematically fix geometry in space. They also can specifically relate one element to another and serve as visual feedback to the user on what these relationships are. After Constraints are created, they are easily modified by merely changing their values or placement. From the ease at which Constraints may be modified and from the inherent downstream associativity of V5, the user can quickly explore alternative designs. Movement of 4 Unconstrained Lines Copyright DASSAULT SYSTEMES 2002

What are Geometric and Dimensional Constraints ?
Geometric constraints A Geometric constraint is a specification of how two geometric elements are related to one another: are the elements coincident (located at the same place), are they concentric, tangent, perpendicular or parallel to one another? Geometric constraint (here concentricity) Dimensional constraints A Dimensional Constraint, one type of Geometric Constraint, specifies the distance between two elements. This distance can be specified as a linear distance, an angular distance, or a radial distance depending on the type of geometric elements involved Dimensional constraint (here distance) Copyright DASSAULT SYSTEMES 2002

What Does Sketching in Context Mean ?
Sketching in context is using existing geometry to create new geometry When sketching with CATIA V5 space geometry is visualized. You can use it to guide your sketch From rough to precise sketch At first, the sketch has to only be made to conform to the spatial intent i.e. the left or right of a hole, on the inside or outside of a pocket, on the top or bottom of a pad, etc. Later, the exact dimensions or precise geometric constraints (concentricity, parallelism, coincidence...) can be applied to the sketch (or profile) to define it precisely 3D geometry used to sketch and constrain profiles Copyright DASSAULT SYSTEMES 2002

You can add constraints between the active sketch and any part edges, vertices or other sketches.
Sketching in Context 1 Activate the Constraint icon 2 Select the edge of the part then the segment to be constrained 3 Select the Distance constraint from the contextual menu (MB3) 4 Place the constraint and modify it if necessary Copyright DASSAULT SYSTEMES 2002

Quick Constraints Dimension Constraints Contact Constraints

Why Quick Constraints? Dimension constraints and Contact constraints are frequently used. Hence, they are made accessible with just one click. Other constraints are chosen from a Constraint Definition Box Copyright DASSAULT SYSTEMES 2002

Setting Dimensional Constraints
3 Select location of dimension 2 1 Select the Constraint icon Select the line to constrain (dimension) Select the Constraint icon 3 4 Post selecting the circle produces a diameter dimension... 5 …but then selecting the line turns the dimension to a distance dimension Pre and post selection affects the way CATIA applies dimensional constraints. Copyright DASSAULT SYSTEMES 2002

Setting Contact Constraints
2 Select the two elements to be constrained Select the Contact Quick Constraints icon 1 Generally, the first selected element will remain in its current position. The second one will move. For more control, use the Fix Constraint beforehand. Copyright DASSAULT SYSTEMES 2002

Modification of Constraints

What Type of Modification Can be Done on Constraints?
All geometric and dimensional constraints may be deleted using the Contextual Menu (third mouse button) Values of dimensions may be changed by double-clicking on them The location of dimensions and the extension lines can be modified by dragging with the left mouse button The type of Constraints applied on an element can be modified by reentering the Constraints Dialog Box and making modifications there A geometric or dimensional constraint attached to an element (i.e. line, circle etc …) can be reconnected to a different element. The geometry will change to conform to the new Constraint setup Copyright DASSAULT SYSTEMES 2002

Modification in the Constraint Dialog Box
1 Select the two lines linked with the Perpendicularity constraint 2 Select the Constraint Dialog Box icon 4 Select a new constraint eg. Verticality Deselect the Perpendicularity check box 3 5 Click OK to Exit Copyright DASSAULT SYSTEMES 2002

Reconnecting a Constraint
1 Double Click on the Tangency Constraint 2 Click on More 6 Click OK to save and exit 5 Select the unassociated line in the Sketcher window 3 Select the Line component 4 Select Reconnect 4 3 Copyright DASSAULT SYSTEMES 2002

Additional Information ...
Dimension value: To modify the position of a dimension's value: Click the icon Select the value text of the dimension Drag the value text to the new position Dimension line: To modify the position of the dimension line: Click the icon Select the dimension line Drag the line to the new position Copyright DASSAULT SYSTEMES 2002

What is Auto-Constraint?
The AutoConstraint Tool: The AutoConstraint tool automatically detects possible constraints between selected elements and imposes these constraints once detected Elements to be constrained Fixed Elements (Independent elements from which other elements can be constrained from - normally the Sketcher Axes) Symmetry Lines (If selected will cause Symmetry Constraints to be created between elements symmetrical to these lines - the symmetry lines themselves will not be constrained) Copyright DASSAULT SYSTEMES 2002

Auto-Constraints 1 Multi-Select the lines in this closed profile. Select the Auto-Constraint Icon 2 3 Select the elements to be constrained 4 Select the Reference Elements Field then select the Vertical and Horizontal Axes 5 Click OK to create the Constraints Auto-Selection tools such as Auto-Search and Trap can be helpful Copyright DASSAULT SYSTEMES 2002

Animating Constraints

What is Animating Constraints?
The Animate Constraint Tool: The Animate Constraints tool allows you to see how a constrained system reacts when you decide to make one constraint vary. In this way, it is a tool for understanding the limitations imposed on the geometry by the current set of constraints. It can be a very useful tool for exploring design alternatives. Copyright DASSAULT SYSTEMES 2002

Animating Constraints
1 Select the dimension you would like to vary 2 Select the Animate Constraint Icon 3 Input the initial and final values and the number of intermediate steps to display 4 Press the Play button. Cancel when done The Animate Constraint panel works like a tape-recorder panel. The user can play forward and backwards, rewind, or play in cyclic repeat mode. Copyright DASSAULT SYSTEMES 2002

Sorting Sketches by their Solving Status
You will see how to sort Sketches by their Status (Under-Defined, Well-Defined, Over-Defined and Inconsistent). Copyright DASSAULT SYSTEMES 2002

What are Sketch Status? You can define four Status for a Sketch : the Under-Defined, Well-Defined, Over-Defined and Inconsistent Status. It is now possible to sort Sketches by their Status. Well-Defined Under-Defined Inconsistent Over-Defined Copyright DASSAULT SYSTEMES 2002

Sorting Sketches by their Solving Status (1/3)
Select “Search” in the Edit Menu. 2 A Dialog box appears and a new attribute “Solving Status” is added to sort Sketches by their Status. 3 Select the Status you want to sort. In our example, we choose the Over-Defined Status. Copyright DASSAULT SYSTEMES 2002

4 After clicking on ‘Search’, the Sketch which is Over-Defined appears in the Dialog box. Copyright DASSAULT SYSTEMES 2002

5 This Sketch is also highlighted in the specification tree and in the geometry area. Copyright DASSAULT SYSTEMES 2002

Relations Between Dimensions

What are Relations Between Dimensions?
Dependencies can be established between dimensions (For example, A=B+C/2) Originally a part of the Knowledgeware set of products, this functionality has been incorporated into the V5 infrastructure and is generally accessible from all Workbenches. In CATIA V5, in addition to relationships between dimension values, dimensions can be made dependent on other parameters such as Forces, Temperature, Time, or Material Properties etc ... Copyright DASSAULT SYSTEMES 2002

Creating a Relation Between Dimensions
1 Select the dimension you would like to be made dependent 2 Use the Contextual Menu (third mouse button) and drag down to Edit Formula 3 1) Select the 40 dimension 2) Type in “+” 3) Select the 10 dimension 4) Type in “/2” When required, open “(“ and Close “)“ parentheses can be used to indicate the order of evaluation for the expression Select OK to create the relation 4 Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have learned:
What Constraints are and what they are used for ... And you have learned how to apply Constraints using: Quick Constraints Constraint Dialog Box Auto Constraint You have learned how to analyze a constrained system using: Animate Constraint and How to sort Sketches using their Solving Status How to establish a relation between Dimensions on a Sketch Copyright DASSAULT SYSTEMES 2002

Managing Sketches Creating Planes Replacing a Sketch
In this lesson you will see: Creating Planes Replacing a Sketch Changing a Sketch Support Sketch Analysis Changing Body To Sum Up Copyright DASSAULT SYSTEMES 2002

Creating Planes You will learn how to create Planes in 3D space to be used as sketching planes Planes Copyright DASSAULT SYSTEMES 2002

Why Creating Planes ? Offset planes Angled planes
Sometimes you will need to create Planes to use them as Sketching planes Offset planes Angled planes Offset planes are used to help define the extrusion extent of a Sketch-Based feature Angled Planes are used to define Sketch-Based features that are angled with respect to other features Offset planes Angled planes Copyright DASSAULT SYSTEMES 2002

Creating an Angled Plane
1 Select the Plane Icon (Available from the WireFrame&Surfaces (WFS or the Generative Shape Design (GSD) Workbenches) 2 For “Angle to Plane” creation type, select edge as reference to rotate resulting plane about 4 The resulting plane (Plane.3) is 45deg to the face, rotated about the selected edge Select the upper face as the reference plane to rotate from. A preview plane that can be dragged to a new location is shown 3 “Angle to Plane” is just one of many creation types possible. Copyright DASSAULT SYSTEMES 2002

Creating an Offset Plane
2 1 Select a Face Select the Plane Icon (Available from the WireFrame & Surfaces (WFS) or the Generative Shape Design (GSD) Workbenches) 3 The offset distance from the reference face can be set by typing the value in the dialog or dragging the circular “handle” on the graphic screen “Offset from Plane” is just one of many creation types possible. Copyright DASSAULT SYSTEMES 2002

Additional Information ...
Different types of plane: The plane definition dialog box provides you with various methods to define planes: Different planes Copyright DASSAULT SYSTEMES 2002

Replacing a Sketch You will learn how to replace a sketch used to support a Solid or a Surface element by a different one Copyright DASSAULT SYSTEMES 2002

Why Replacing a Sketch ? Replacing a sketch is a quick way to modify solids or surfaces using that sketch for their definition. The user creates a new sketch with a new profile. This new sketch will replace the old one. The solids or surfaces that are based on the previous sketch do not have to be re-created. They will be modified automatically. Copyright DASSAULT SYSTEMES 2002

Replacing a Sketch 3 Right click on the original sketch and drag down to “Replace”. Click on your new sketch as the replacing sketch 2 Create the new sketch on the same plane (Note: although this is normally the case - it is not a requirement) 1 Check which plane the original sketch lies on. You can use the Parent/Children analysis from the Contextual Menu (third mouse button on the sketch) if you like 4 Copyright DASSAULT SYSTEMES 2002

Changing a Sketch Support

Why Changing a Sketch Support?
By changing its supporting plane, a sketch can be moved to a new plane without having to recreate it Copies of a sketch can be moved onto different planes in this way Copyright DASSAULT SYSTEMES 2002

Changing the Sketch Support
1 While outside the Sketcher mode, use the Contextual Menu on the Sketch to be modified and drag down to Change Sketch Support Any Solid or Surface elements attached to the Sketch will be moved accordingly 2 Select the new plane for the Sketch Copyright DASSAULT SYSTEMES 2002

Sketch Analysis You will learn how to analyze sketches: geometry, projection and intersection. You will get either a global or an individual status, and you will be able to correct any problem Copyright DASSAULT SYSTEMES 2002

Why Analyzing the Geometry of a Sketch? (1/2)
Most of the time, you draw a sketch in order to use it to build sketch based features (e.g. pads). Sometimes, when you try to use a sketch, CATIA refuses to build the feature because the sketch is not closed (or overlapping) and it is sometimes difficult to see where the sketch is opened (or overlapping). The Tools + Sketch Analysis option allows you to check whether a sketch can be used to create a sketch based feature Copyright DASSAULT SYSTEMES 2002

Why Analyzing the Geometry of a Sketch? (2/2)
During the sketch analysis, it is possible to do corrective actions: Set in Construction Mode Close Opened Profile Delete Geometry Copyright DASSAULT SYSTEMES 2002

Why Analyzing the Projection/Intersection of a Sketch? (1/2)
The Sketch Analysis option can be used to check the projection onto or intersection with 3D elements Copyright DASSAULT SYSTEMES 2002

Why Analyzing the Projection/Intersection of a Sketch? (2/2)
During the sketch analysis, it is possible to do corrective actions: Isolate Geometry Activate / Deactivate Delete Geometry Replace 3D Geometry Copyright DASSAULT SYSTEMES 2002

Analyzing a Sketch: Geometry (1/2)
The Tools + Sketch Analysis command allows you to check if a sketch can be used to create a sketch based feature In order to edit the sketch, double click on Sketch.1 in the tree 1 2 Select the Tools+ Sketch Analysis menu option Copyright DASSAULT SYSTEMES 2002

Analyzing a Sketch: Geometry (2/2)
The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature 3 If necessary, select the Geometry tab in the dialog box 4 In order to better see the sketch, select the Hide constraints button, the constraints will be hidden You can now see where the sketch is opened and you can correct it Copyright DASSAULT SYSTEMES 2002

Analyzing a Sketch: Projection/Intersection (1/2)
The Tools + Sketch Analysis menu option allows you to check if a sketch can be used to create a sketch based feature In order to edit the sketcher, double click on Sketch.3 in the tree 1 2 Select the Tools+ Sketch Analysis menu option Copyright DASSAULT SYSTEMES 2002

Analyzing a Sketch: Projection/Intersection (2/2)
The Tools + Sketch Analysis menu option allows you to check if a sketch can be used to create a sketch based feature 3 If necessary, select the Projection/Intersection tab in the dialog box 4 You can now check if the intersections and projections contained in the sketcher are valid or not Intersection between 3d elements Projection of 3d elements Copyright DASSAULT SYSTEMES 2002

Different corrective actions can be done when analyzing a sketch: Analyzing a Sketch: Geometry Set in Construction Mode Close Opened Profile Delete Geometry Copyright DASSAULT SYSTEMES 2002

Different corrective actions that can be done when analyzing a sketch: Analyzing a Sketch: Projection/Intersection Isolate Geometry: When using this icon, the selected projected or intersecting element is separated from its 3d components Activate/Deactivate: When using this icon, the selected element (of the sketch) is no more taken into account when creating a sketch based feature, but the element still exists Delete Geometry: When using this icon, the selected element is remove from the sketch Replace 3d Geometry: When using this icon with a projected or intersecting element (intersection or projection with 3d objects), you can select another 3d element to modify the projection or the intersection Copyright DASSAULT SYSTEMES 2002

You will learn how to move one sketch from a body to another one
Change Body You will learn how to move one sketch from a body to another one Copyright DASSAULT SYSTEMES 2002

Why Moving One Sketch from a Body to Another one ?
When working with several bodies, you may want to create a sketch based feature (a pad for example) and the necessary sketch has been created in a body different from the active one. In this case you may want to transfer the sketch from its body of creation into the active one (it is not mandatory but it is helpful to understand the part structure Copyright DASSAULT SYSTEMES 2002

Changing Body 2 1 You can move one sketch from a body to another one
Select the body in which you want to move the sketch, then select OK 2 1 Select the Change body command from the sketch contextual menu You get: Copyright DASSAULT SYSTEMES 2002

To Sum Up ... You have learned how to manage 2D sketches in 3D space by: Creating Planes in 3D and using tools such as: Replacing a Sketch Changing a Sketch Support Sketch Analysis Copyright DASSAULT SYSTEMES 2002

Sketcher CATIA Training Foils Version 5 Release 9 June 2002

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Sketcher CATIA Training Foils Version 5 Release 9 June 2002

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